Should I use a Conformal Mesh (Shared Topology) or a Non-Conformal (Bonded Contact) Mesh in my Analysis?
January 25, 2023 at 7:34 amFAQParticipant
In a multi-body part, a conformal mesh ensures that the nodes on both sides of the interface matches. With a non-conformal mesh, the nodes on one side of the interface does not match the nodes on the other side of the interface. The reason why conformal meshes is preferred over non-conformal meshes: with a conformal mesh there is no (or very little) interpolation at the interface which therefore reduces computational time and ensures higher accuracy of the solution. One way to review the results of a non-conformal mesh is to request a Directional Displacement scoped to the two parts. Zoom in on the surface that has the bonded contact. On the legend, grab the line that separates red from the color below and drag it down until red fills one of the parts with red and back off a little so there is a couple of colors leading up to the bonded surface. Now grab the line that separated blue from the color above and drag it up until blue fills one of the parts and back off a little so there is a couple of colors leading up to the bonded surface. You have just created a very sensitive colormap to see displacement discontinuities across the bonded interface. If you had a conformal mesh, the displacements must be continuous across the interface because there is a shared node. If the bonded contact allows some relative motion, you will see a step in the displacement contour. You can use the colormap to quantify the size of the step. In most cases, the first recommendation is to use Shared Topology instead of bonded contact (even) because depending on which formulation is used, there can be some shear flexibility added by the contact element. Two reasons a conformal mesh might not converge when a non-conformal mesh did converge is if the element size was larger on the conformal mesh, or if the element quality was worse on the conformal mesh. When I have two bodies of different materials that move together because they are bonded, I first choose shared topology, which creates a conformal mesh, and let the two bodies be connected to the same nodes shared on the common face. If I want to study the stress in the bonded interface, then I change to bonded contact where I have more options for that study. I say two bodies of different materials because if they are the same material, then I could unite them in CAD. Sometimes you can get a better quality mesh by splitting a single body into multiple bodies that are easier to mesh and use shared topology to connect them.
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- The warning message is: “The maximum contact stiffness is too big. This may affect the accuracy of the results.” Why does large contact stiffness affect results accuracy?
- Contact Definitions in ANSYS Workbench Mechanical
- After Workbench crashes, how can I recover the project from a .mechdb file?
- Model has a large number of contacts – how to reduce them?
- How to resolve “Error: Invalid Geometry”?
- How to deal with “”Problem terminated — energy error too large””?”
- How to display the color of each body based on the material in Mechanical?
- The LS-DYNA equivalent of *MODEL_CHANGE card (in ABAQUS). Which keywords can be used to introduce(activate)/delete(deactivate) elements in the middle of a calculation (at user-specific time/load steps).
- How to locate an element of a particular ID number in Mechanical?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
© 2023 Copyright ANSYS, Inc. All rights reserved.